Referencing current geometry while sketching a section

[jrinad70]

Ok, this is driving me crazy.  I have a simple cylinder 10 mm is diameter and 40mm long.  I want to revolve a simple cut around the cylinder.  I selected a datum plane that goes through the axis of the cylinder (had to create an axis first, not sure why Fusion doesn't automatically create an axis through cylinders on its own when a cylinder is created) as a sketching plane for a sketch.  I'm in the sketching environment.  I sketch a rectangle I'll revolve later for a cut.  I dimension the rectangle's location 18 mm from the bottom of the cylinder.  Here is where I run into two issues.

1) Dimensioning the ID of the rectangle.  Fusion will let me create a radial dimension from the inside edge of the rectangle to the center of the cylinder.  I want a diameter dimension (3.5 mm).  How do you create one?

2) How does one make the outside edge coincident with the cylinder edge so if the diameter of the cylinder changes the cut will automatically follow?  Fusion will not let me select the edge of the cylinder to align my sketching line to it.

Illustration of problem (I had to create the example is Creo because I didn't have access to Fusion while creating the post).

[jeff_strater · Accepted solution]

1. Diameter dimension is available on the context menu during the dimension command

2. Use the Project command, with type set to Bodies to get the silhouette edge

screencast:

[jrinad70]

Jeff,

thanks for this!  That definitely works.  Seems like a lot of work though.  Why can't one just draw the rectangle, pick the coincident tool, click on the edge of the cylinder (creating a reference) and then the line on the rectangle having it then just snap the rectangle's edge to the reference.?  Currently one has to initiate another command that creates lines of the entire x-section of the cylinder!?  That was three extra section lines in the section that aren't needed and just sever to clutter up the section (of course this was a simple example so not that big of a deal).  I guess I would then go ahead and delete the three extra lines and turn the one I needed into a construction line just to help clean up the section (more work).  And what's with having to draw yet another line just to create the diameter dimension?  It's these simple tasks that gets me so frustrated with Fusion.  If they would fix these kind of things other software wouldn't be able to compete.  Anyway, I'm ranting.

Thanks again for taking the time to show me the resolution I do appreciate it!

[jeff_strater]

That's good feedback, @jrinad70, you raise some good points here - it certainly could be easier, I agree.

A couple of comments:

• "pick the coincident tool, click on the edge of the cylinder (creating a reference)".  That, in fact, is part of the problem - there is no edge there - it's just a continuous face all the way around.  In order to get the line that you need, you need to do one of these "silhouette edge" projections.  As to whether we should automatically do that projection, I think that might be one of those "be careful what you ask for" things.  You would get a lot of silhouette edges being projected into your sketch.  It could lead to a cluttered sketch, and create references to geometry that you don't really need.  Still, I agree, there is room for ease-of-use improvement here.
• "And what's with having to draw yet another line just to create the diameter dimension?"  A valid point, I agree.  Personally, I like having that line in there, so I don't mind creating it.  Normally, I would make it construction to de-clutter the sketch
• We are working on a change to allow you to create construction geometry directly from the Project command.  This should be out soon, but might not make the very next update.  This will help save one step if you want the projected geometry to be construction

[jrinad70]

Jeff,

thanks for the reply.

• concerning "be careful what you wish for".  I understand where you're coming from as features that are intended to "help out" can lead to problems down stream.  But, in this case I don't think so.  I've been using Creo (Pro/Engineer) now as a design engineer for 30 years.  Creo does the very thing I described.  When in sketch mode, I can click on the coincident constraint and click on the "edge" of the cylinder and it instantly creates a reference line which I can then align sketched entities to.  For sure this can get one in trouble if one doesn't understand the parent-child relationship it's creating, but it is "parametric modeling" after all.  However, in situations such as my example, it is a relationship I want.  In my mind it should be up to the user to determine when or when not to create that relationship, not the software.  Here's the catch though, a parent-child relationship was still created via using the project command.  In fact, it was worse because it created four edges with a parent-child relationship instead of just the one I would have created by clicking the single "edge".
• Point number two.  I don't have a problem with creating a centerline to create the diameter dimension.  In fact, in Creo when creating a revolved feature I have to create a centerline which becomes the axis of revolution for the feature.   So, either way, a line has to be created.
• I think allowing construction lines to be created from the project command is on the right track.  I would take it a bit further though and do as follows.  Create a new sketching command (located in the sketching pallet) called "References".  After a users selects it he would then be able to select any edge (even silhouette edges) from existing geometry,  any construction plane or construction axis and it would create a construction line/arc/circle of infinite length (if a line).  Then another new geometry to sketch would snap to it when drawing.

I have another compliant/feedback on another basic sketching function but instead of putting it in here, I'll create a new entry when I get the chance.

[thomas.vanek]

For future reference, when someone else stumbles upon this post/problem:

Solution for me was to activate "Auto Project edges on reference" in the Preferences unter General -> Design